Dimensional compensation for FDM holes

Every hole in a printed part needs a decision: do you model it at nominal size and rely on the slicer, or do you deliberately oversize it in CAD to counter the undersizing described in the pillar guide of this cluster. In our experience the second approach is the only one that gives repeatable results across a production run, but it has to be done with the right numbers for the right material, not as a single blanket rule applied to every hole in the part.

How much to oversize and why

The undersizing a hole experiences comes from a combination of nozzle width, extrusion flow calibration, and, for horizontal holes, sag. For a vertical hole in the 3 to 12 mm range printed with a 0.4 mm nozzle, a compensation of 0.2 to 0.3 mm added to the diameter is a reasonable starting point on PLA and PETG. On ABS and ASA, where cooling shrinkage adds a bit more, 0.3 to 0.4 mm is more typical. Very small holes, under 3 mm, sometimes need proportionally more compensation because the perimeter has less room to absorb the rounding error.

These are starting values, not universal constants. Nozzle wear, flow rate calibration and even ambient temperature in the print room shift the numbers slightly. For parts with a genuinely critical fit we recommend printing a small test coupon with a range of hole sizes and measuring the result before committing to a production run, rather than trusting a table blindly.

Compensating in CAD versus at the machine

Some slicers offer a global hole horizontal expansion setting that scales all circular negative features by a fixed amount. This can help but is a blunt instrument: it applies the same offset to a 3 mm pin hole and a 20 mm bearing bore, even though the ideal compensation differs between them. It also does not distinguish between a clearance hole that needs generous compensation and a press fit hole that needs almost none.

Our recommendation is to model each functional hole at its intended final diameter, adding the compensation directly in CAD based on its role, clearance, press fit or slip fit, rather than relying on a single slicer-wide setting. This keeps the model self-documenting: anyone opening the file later sees the actual intended print diameter, not a nominal value hiding an invisible global offset.

Why blanket oversizing breaks press fits

A press fit hole for a bearing or bushing is designed to be slightly smaller than the outer diameter of the part it receives, so that the printed material grips it. If a blanket compensation rule adds 0.3 mm to every hole in a part regardless of function, a press fit bore that was meant to be 0.1 mm undersize suddenly becomes 0.2 mm oversize, and the bearing simply falls out. This is one of the most common mistakes we see in files that come to us after a first print run failed.

The fix is straightforward once you separate hole types. Clearance holes get generous compensation because a loose fit there costs nothing functionally. Press fit holes get little or no compensation, and are often modelled undersize on purpose. Slip fit holes for pins or shafts sit in between, usually 0.1 to 0.2 mm larger than the shaft diameter after compensation.

Nominal versus modelled diameter for common fasteners

For clearance holes on screws and dowel pins, the table below gives modelled diameters we typically use as a starting point on PLA, PETG and carbon-filled materials with a 0.4 mm nozzle, on vertical holes. These are close fits suitable for general assembly, not free-running clearance. For a looser fit, add another 0.1 to 0.2 mm.

These values assume a well calibrated machine and are a starting point for a DFM discussion, not a substitute for measuring a first article on a critical assembly. Every material and machine combination drifts a little differently, which is exactly why we validate fits during sample production before a series order goes ahead.